Post Go back to editing

ADSP-2148x E-pad question


I have just finished reading the EE- 352 Engineering note regarding E-pad packages and mounting techniques. One thing I am not clear of is you don't say whether or not you use thermal relief's or direct connects on the ground plane connecting via's. Obviously direct connection would give you better electrical connection and lower thermal resistance to the ground plane but would it alter the temperature profile needed for reflow ? ie which would be better from the point of view of manufacturability ?



  • Thanks Al

    How big is the center hole that you use ?

    I have made provision for a 5 mm hole in the middle of the pad so I can solder it. I also did what they have suggested in EE-352 and used an outer perimeter of small vias and tent them using solder mask.

    Do you think the large hole could be left in the production units even if most of the paste drops into the hole ? I don't mind having to rework the board after they go though production. According to EE-352 you need to experiment with the temp profile and amount of paste until you minimize the number of solder voids under the pad. Sounds like a hit and miss process to get it right and unless you have an xray machine how would you know ? I like the idea of the large pad hole do I can make sure it is done right which is why I asked about thermal reliefs because I know that soldering to a pad directly connected to a plane can be a bit tricky as the plane soaks up all of the heat from the iron.  However that could work in favour in order to minimize heat stress on the chip.

    Also the switcher IC I am using ADP2323 recommends that I bake the chip at 120 degrees C for 24 hours before reflow. Is this really neccessary if I hand solder the chip onto the board ?



  • I always use many multiple direct connects. You want the impedance to be very low.

    On some boards, I also use a large center hole as well. This makes prototyping and rework easier in cases where you are not going to have an automated reflow. The stencil will apply paste in four quadrants, so that it doesn't go into the center hole.

    If the profile is set up correctly, you will not have a soldering issue.

    BTW, The same issue applies to many buck regulators used for the core supply - No reliefs.

    Al Clark

  • I use a 2.2mm center hole. This is sufficient for hand soldering. A 5mm hole is much too big.

    On the 100 pin 21489, I used 24 sounding vias with 0.2mm holes

    For hand soldering, we start with a small heater, Hakko FR-830. This preheats the board for better solder reflow.

    It is possible to use solder, but we usually opt for paste. We solder a few outside pins on the LQFP first to insure alignment, and then use either a good iron or hot air.

    A similar process is used for switchers. These are actually a little more difficult. Layout is critical for switchers. There is a small triangle area that includes the switch, inductor and output capacitor that should be very low impedance as well as the high current grounds.. You also want to avoid noise on the voltage divider and compensation. Read the datasheet many times and look at similar devices. They all have similar layout issues.

    The ADI ADP2119 or ADP2120 is excellent for the core. It eliminates the need for external FETs.

    Of course, all these hand soldering tricks are less than ideal compared to using a stencil and reflow. It's OK for prototyping, etc. but not what I would want to do in production.

    We have never had a process problem with 21489 or 21479 devices in production. The profile is not that special. Any good contract manufacturer should get it right.

    I have never heard of preheating parts for 24 hours before using. I doubt it a real big issue.

    Al Clark

  • Hello Al

    Regarding the 2mm hole how do you solder it ? Do you plug up the hole with solder paster and hit it with a hot air gun until it reflows or do you use a narrow tip, heat up the hole a bit and then feed in solder into the hole ? If you use a soldering iron what size tip and temperature do you use ?



  • We apply paste to the pad before we place the part.

    I think hot air works better than an iron. If the small vias are not completely covered by the mask, you can see some outgassing which helps you know you are melting the solder.

    I should point out that I don't actually do any of this myself. I have skillful people. This means that this is the method I observe, but I could be a little off on the details. I know the hole size is correct since I lay out the PCBs.


  • Hello,

    I have designed my custom board with a ADSP-21489 (176 lead package) and I am having a problem with EPAD. After solder it on my board I was checking for short circuits and i found one between GND and VDD_INT (internal supply for ADSP). I removed the DSP and check the short circuit again and no problems found. Then I solder back the DSP and the short circuit is back.

    Since I have 2 DSPs I decide to check the connection between EPAD and GND. I verified something strange. The EPAD seems to be connected to VDD_INT pins and have no connection to GND pins. Is it normal?

    ADSP datasheet says that EPAD must be connected to GND.

    Best Regards,


  • Hello Pedro

    Which VDD_INT pins are you measuring the short with the EPAD ?

    Also there are two ground pins (15 and 109) that should be connected to ground. Perhaps you have connected one of these to VDD_INT on your board ?



  • Hello David,

    Thanks for your answer. I tested the connection between every pin of DSP. In fact it have 50Ohm (approximately)  impedance between pins.

    I took the risk and power it on, and it works well. Maybe it is normal..



  • Pedro was confusing low resistance with "short"

    The impedance between Vint and GND will be low since this is where all nearly all the current draw will be.

    If the part was drawing 500mA, which is not actually the case at reset, etc, then 1.1V/500mA = 2.2 ohm

    Al Clark

  • Thanks for your answer Al. I didn't think about that.